CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Bugs

SetField problem in OpenFoam 14

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 13, 2007, 05:14
Default hi I am trying to re-run a
  #1
New Member
 
Joakim Möller
Join Date: Mar 2009
Posts: 26
Rep Power: 7
joakim is on a distinguished road
hi

I am trying to re-run a case that I ran in OpenFoam 1.3. When using the setField function, I get the following output on the screen:


Create mesh for time = 0

#0 Foam::error::printStack(Foam:stream&)
#1 Foam::sigFpe::sigFpeHandler(int)
#2 ??
#3 Foam::wedgePolyPatch::initTransforms()
#4 Foam::wedgePolyPatch::wedgePolyPatch(Foam::word const&, Foam::dictionary const&, int, Foam::polyBoundaryMesh const&)
#5 Foam::polyPatch::adddictionaryConstructorToTable<f oam::wedgepolypatch>::New(Foam ::word const&, Foam::dictionary const&, int, Foam::polyBoundaryMesh const&)
#6 Foam::polyPatch::New(Foam::word const&, Foam::dictionary const&, int, Foam::polyBoundaryMesh const&)
#7 Foam::polyBoundaryMesh::polyBoundaryMesh(Foam::IOo bject const&, Foam::polyMesh const&)
#8 Foam::polyMesh::polyMesh(Foam::IOobject const&)
#9 Foam::fvMesh::fvMesh(Foam::IOobject const&)
#10 main
#11 __libc_start_main
#12 __gxx_personality_v0 at ../sysdeps/x86_64/elf/start.S:116
Floating point exception


The domain is an axi-symmetric case but the collapsed surface is replaced by a finite-area surface. What have changed in the setField-function?

regards

/Joakim
joakim is offline   Reply With Quote

Old   April 13, 2007, 05:19
Default Is the case small enough to po
  #2
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
Is the case small enough to post here for us to test or if not can you make a small case which reproduces the problem?

Henry
henry is offline   Reply With Quote

Old   April 13, 2007, 09:51
Default Dear Henry I have construct
  #3
New Member
 
Joakim Möller
Join Date: Mar 2009
Posts: 26
Rep Power: 7
joakim is on a distinguished road
Dear Henry

I have constructed two tar-files for the v1.3 and v1.4.

Regards

/Joakim




joakim is offline   Reply With Quote

Old   April 13, 2007, 10:34
Default Sorry! I can't upload the f
  #4
New Member
 
Joakim Möller
Join Date: Mar 2009
Posts: 26
Rep Power: 7
joakim is on a distinguished road
Sorry!

I can't upload the files, they are too big.

To be a little more desciptive instead:
I generated a mesh in i Icem-tetra, which was saved in star-format and converted via starToFoam. The domain in L-shaped with an inlet at the top and wedge-conditions on the sides. Remaining b.c. are pressure-outlet and wall.

I did some more testing I have found out that the problem is not with setField. I ran checkMesh on the mesh and this one failed for the v1.4 too with an output that is vey similar to the one I got whenI ran setField:


Create polyMesh for time = constant

#0 Foam::error::printStack(Foam:stream&)
#1 Foam::sigFpe::sigFpeHandler(int)
#2 ??
#3 Foam::wedgePolyPatch::initTransforms()
#4 Foam::wedgePolyPatch::wedgePolyPatch(Foam::word const&, Foam::dictionary const&, int, Foam::polyBoundaryMesh const&)
#5 Foam::polyPatch::adddictionaryConstructorToTable<f oam::wedgepolypatch>::New(Foam ::word const&, Foam::dictionary const&, int, Foam::polyBoundaryMesh const&)
#6 Foam::polyPatch::New(Foam::word const&, Foam::dictionary const&, int, Foam::polyBoundaryMesh const&)
#7 Foam::polyBoundaryMesh::polyBoundaryMesh(Foam::IOo bject const&, Foam::polyMesh const&)
#8 Foam::polyMesh::polyMesh(Foam::IOobject const&)
#9 main
#10 __libc_start_main
#11 __gxx_personality_v0 at ../sysdeps/x86_64/elf/start.S:116
Floating point exception

As before, checkMesh for v1.3 did just fine.

Regards

/Joakim
joakim is offline   Reply With Quote

Old   April 13, 2007, 11:08
Default Hi Joakim, Is your case act
  #5
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
Hi Joakim,

Is your case actually 2D? Wedges will only work on 2D cases (i.e. 1 cell thick, created/createable by rotational extrusion). So it will not work with e.g. tetrahedra. The checking in 1.4 is a bit more strict than in 1.3.
mattijs is offline   Reply With Quote

Old   April 14, 2007, 06:06
Default Hi Mattijs Yes it is a 2D c
  #6
New Member
 
Joakim Möller
Join Date: Mar 2009
Posts: 26
Rep Power: 7
joakim is on a distinguished road
Hi Mattijs

Yes it is a 2D case. One layer of tetras extruded to a prisms layer.

The reason I worked with the case is that I never got O.F. v1.3 to accept the genuine 2D-axisymmetric meshes created in icem-tetra.
We had a discussion about this onces under the thred "Axisymmetric bodies, wedge-type B.C.'s". You came up with a suggestion to use the collapseEdges utility, but since my mesh doesn't contain quads I guess this approach doesn't help.

As I stated back than, I constructed two meshes. One structured mesh using blockMesh and an unstructured mesh in ICEM-tetra. I noted a difference when running checkMesh on the two cases. For the structured mesh, in the output, it writes out empty when it checks the collapsed surface, whereas in the case of the unstructured mesh it complains that the surface area is 0. I assume the same goes for the solver. The code ignores the empty boundary in the blockMeshed-case where the empty b.c. is accepted, whereas the OpenFoam still thinks by 2D-axisymmetric mesh is a 3D mesh with an empty b.c. which is not tolerated and the solver fails to start.

I have not tested the unstructured mesh in v1.4 yet but I will do that as soon as I can. The structured mesh I mention above worked fine.

Regards

/Joakim
joakim is offline   Reply With Quote

Old   April 14, 2007, 08:16
Default Can you create a small unstruc
  #7
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
Can you create a small unstructured testcase which shows the problem and you can send over? The collapseEdges should collapse the zero-area axis faces.
mattijs is offline   Reply With Quote

Old   April 24, 2007, 09:20
Default Dear Mattijs Sorry for the
  #8
New Member
 
Joakim Möller
Join Date: Mar 2009
Posts: 26
Rep Power: 7
joakim is on a distinguished road
Dear Mattijs

Sorry for the delayed repsons. I have created two very small test-problems. The first case is a wedge-shaped domain with a collapsed interface, see image



The second test case as a geometry with the same shape but the collased interface is replaced with a surface with a small area.



The first problems works in neither O.F 1.3. or O.F 1.4 whereas the second problem works in O.F 1.3.

This is what I did in O.F.1.4:

The meshes where created in icem-cfd v.11. Saved into star-format and translated via starToFoam to O.F-format. The starToFoam application seems to run fine, but when doing checkMesh I get the following outputs

case1: log_before

case2: log_before_2

Note how it complains about the elements with 0-area surface. If we just go a head and run FoamX to subscibe bounday conditions, where the sides are given wedge-bounday conditions and running checkMesh afterword both cases fails. This did NOT happend using O.F. 1.3

case1: log_after

case2: log_after_2

I conclude that here are to problems
1) The seems to be something wrong with the wedge-condition. This part worked in O.F. 1.3.
2) As I stated ealier when I ran a similar geometry with a mesh constructed in blockMesh, checkMesh noted that the collapsed bounday had an empty b.c. and ignored it, so did the solver.
For the icem-tet mesh, checkMesh do not ignore the boundary, neither the solver whish I assume it should.

I hope a have been clear enough about the problems

Best regards

/Joakim
joakim is offline   Reply With Quote

Old   April 24, 2007, 09:39
Default Can you post the meshes themse
  #9
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
Can you post the meshes themselves so we can have a look? If they're too big to post (> 50k or so) just send them directly to me.
mattijs is offline   Reply With Quote

Old   April 24, 2007, 09:50
Default Hi Mattijs Sorry, I forgot
  #10
New Member
 
Joakim Möller
Join Date: Mar 2009
Posts: 26
Rep Power: 7
joakim is on a distinguished road
Hi Mattijs

Sorry, I forgot to post the cases:

case1: VF_1_14.tar.gz

case2: VF_2_14.tar.gz

Regards

/Joakim
joakim is offline   Reply With Quote

Old   April 24, 2007, 11:41
Default - Switch off FOAM_SIGFPE and 1
  #11
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
- Switch off FOAM_SIGFPE and 1.4 runs through for me.

- Your wedges do not straddle a coordinate plane. Instead one of them is in the xy plane. See section 6.2.2 of User Guide about wedges.
mattijs is offline   Reply With Quote

Old   April 25, 2007, 05:47
Default Hi Mattijs Tnx for your rep
  #12
New Member
 
Joakim Möller
Join Date: Mar 2009
Posts: 26
Rep Power: 7
joakim is on a distinguished road
Hi Mattijs

Tnx for your replay, so I tried what u suggested:

case2:
1) So it seems that by symmetrizing the wedge-mesh around the xy-plane makes things work.

VF_1_14.tar.gz

This was not neccesary in O.F. 1.3. Note that this was regardless the of value of FOAM_SIGFPE. By the way, when you say "turn off", do you mean

export FOAM_SIGFPE=false

in the bashrc file under .OpenFOAM-1.4 ?

2) I did the same symmetrization with case1. Here I still get the problem with the empty b.c.

log_out

and the solver still complain about the 0 face area when I run checkMesh.

Did I do something wrong with FOAM_SIGFPE?
or is this due to something else.

regards

/Joakim
joakim is offline   Reply With Quote

Old   April 26, 2007, 03:43
Default 1) You'll have to unset FO
  #13
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
1) You'll have to

unset FOAM_SIGFPE

Setting it to anything (even 'false') switches on the trapping.

2) empty patches and fields are to be used for front and back of 2D cases. Yours are on the wedge axis if I remember correctly.
mattijs is offline   Reply With Quote

Old   May 16, 2007, 06:51
Default Hi, I got similar problems as
  #14
Member
 
Rolando Maier
Join Date: Mar 2009
Posts: 89
Rep Power: 7
rolando is on a distinguished road
Hi,
I got similar problems as Joakim. My case interrupts with simialar messages as above.
I donīt have wedges in my case but empty patches.
If I unset FOAM_SIGFPE, as Mattijs proposed above, it works.
What does unsetting this variable cause?
Why didnīt I have this problem with OpenFOAM-1.3?

Can anybody tell me something about this?

Rolando
rolando is offline   Reply With Quote

Old   January 31, 2008, 04:09
Default Yes, when I used liftDrag, I g
  #15
Senior Member
 
lakeat's Avatar
 
Daniel WEI (老魏)
Join Date: Mar 2009
Location: South Bend, IN, USA
Posts: 688
Blog Entries: 9
Rep Power: 10
lakeat is on a distinguished road
Send a message via Skype™ to lakeat
Yes, when I used liftDrag, I got the same problems.
again, What does unsetting this variable cause?

Thanks

Daniel
__________________
~
Daniel WEI
-------------
NatHaz Modeling Laboratory
Department of Civil & Environmental Engineering & Earth Sciences
University of Notre Dame, USA
Email || My Personal CFD Blog
lakeat is offline   Reply With Quote

Old   October 30, 2008, 08:51
Default How can I unset FOAM_SIGFPE ?
  #16
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 299
Rep Power: 8
openfoam_user is on a distinguished road
How can I unset FOAM_SIGFPE ?

Which file do I have to modify ?

I have to modify the file .cshrc located in OpenFOAM/OpenFOAM-1.5/etc/ ?

Thanks,

Stephane
openfoam_user is offline   Reply With Quote

Old   October 28, 2009, 09:50
Default Setfield error
  #17
New Member
 
lostin
Join Date: Jul 2009
Location: India
Posts: 12
Rep Power: 7
lostin4ever is on a distinguished road
I am trying to re run a tanksloshing case using latestTime utility for further time. It is showing error (pasted below). Can anybody tell how to get rid of this error.


Create time

Create mesh for time = 2.4

Selecting dynamicFvMesh solidBodyMotionFvMesh
Selecting solid-body motion function SKA

Reading g
Reading field p

Reading field alpha1

Reading field U

Reading/calculating face flux field phi

Reading transportProperties

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Selecting turbulence model type laminar


Unable to set reference cell for field p
Reference point pRefPoint (0 0 0.15) found on 0 domains (should be one)


file: /home/akash/OpenFOAM/akash-1.6/run/multiphase/interDyMFoam/ras/sloshingTank_practice1/system/fvSolution::PISO from line 94 to line 103.

From function void Foam::setRefCell
(
const volScalarField&,
const dictionary&,
label& scalar&,
bool
)
in file cfdTools/general/findRefCell/findRefCell.C at line 93.

FOAM exiting

lostin4ever is offline   Reply With Quote

Old   October 30, 2009, 08:18
Default
  #18
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 15
mattijs is on a distinguished road
Your mesh is moving. You'll have to make sure that the reference point is inside the mesh (upon restart).
mattijs is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
How to use setField to create sphere sega OpenFOAM Pre-Processing 36 February 9, 2013 12:19
How to use SetField tian OpenFOAM Pre-Processing 2 May 18, 2009 04:06
Problem installing OpenFOAM 141 sachin OpenFOAM Installation 2 February 22, 2008 10:20
OpenFOAM 14 compilation problem zaferleylek OpenFOAM Installation 4 May 8, 2007 14:52
Problem compiling OpenFOAM on AIX 53 haunschmid OpenFOAM Installation 1 October 17, 2006 12:58


All times are GMT -4. The time now is 17:38.